What's new
What's new

Slotting with 1/8" cutter, need suggestions on speeds/feeds

SkeeterWeazel

Plastic
Joined
Apr 20, 2021
Beginner CNC machinist here. Trying to cut 1/8" slots in 1/8" cold rolled steel. Not going well.

Using 4 flute carbide EM, 1/4" flute length. 4000 RPM, .042 DOC, .0003 feed/tooth. Based on info from Harvey tool site.

I can ramp in OK, but attempt today the cutter broke after about a 1/4" into slot.

Thinking i need to reduce the DOC. Even with the small feed/tooth the cutter may be loading up? I'm using a mist cooler.

I've had some success with a 3 flute. Maybe it was just luck. Thinking 4 flute should be stronger.

Please give me your suggestions.

Thx.

Marty
 
Beginner CNC machinist here. Trying to cut 1/8" slots in 1/8" cold rolled steel. Not going well.

Using 4 flute carbide EM, 1/4" flute length. 4000 RPM, .042 DOC, .0003 feed/tooth. Based on info from Harvey tool site.

I can ramp in OK, but attempt today the cutter broke after about a 1/4" into slot.

Thinking i need to reduce the DOC. Even with the small feed/tooth the cutter may be loading up? I'm using a mist cooler.

I've had some success with a 3 flute. Maybe it was just luck. Thinking 4 flute should be stronger.

Please give me your suggestions.

Thx.

Marty

If it is a straight slot, can you turn the part 90 degrees and use a carbide slitting saw? Alternatively, use a smaller end mill and an adaptive tool path. This link may be of use. It is slotting with stainless steel with 1/8" end mill: Milling 304 Stainless with a Carbide End Mill | Speeds and Feeds Tool Test - YouTube
 
Yeah, when I read the thread title, I immediately thought slitting saw, which should be reasonably robust at 1/8" width. 0.001" per tooth feed for starters. Whatever SFM is appropriate for the cutter and work materials.
 
Thx for replies. I'm making a router guide plate of sorts, Some slots are curved. After watching video i think i'm not use enough "mist" to flush out chips. I am using a "cheapy" cutter from McMaster Carr. Maybe 3 flute is better. Crap, i hate breaking cutters. If i felt i was learning it wouldn't be so bad. But i feel i'm just shooting in the dark.
 
Thx for replies. I'm making a router guide plate of sorts, Some slots are curved. After watching video i think i'm not use enough "mist" to flush out chips. I am using a "cheapy" cutter from McMaster Carr. Maybe 3 flute is better. Crap, i hate breaking cutters. If i felt i was learning it wouldn't be so bad. But i feel i'm just shooting in the dark.

4 flute is stronger, but less room for chips. Maybe a 2 flute for better chip evacuation. I don't like 2 flutes, but without flood coolant... maybe will be better?
 
Osg 5 flute. If you can program it use a trichordial toolpath. I cut .16” wide .10” deep by 1.50” long slots in 316l at 20 ipm 6200 rpm with a .020 stepover. The end mill will run for hours this way. I use the peel mill feature in mastercam. You can also write a simple macro to do this.
 
If I can I default to high feed milling for situations like this. If not, I'll use a profile ramp with a stepdown limited to around 1/4-1/3 of cutter diameter using a smaller endmill (In this case I'd use a 3mm). I will use a corner radius tool in steel. Chip evacuation is huge - this might sound obvious but make sure you're blowing chips behind the toolpath not in front of it.
 
Some other ideas to try after you reduce the DOC: change material to a leaded steel, like 12L14. If this is a project for your own use, spoil yourself and use brass. Also try the first passes with a ball end mill, then clean up with an end mill. And along the way, learn to make "D bit" cutters, essentially a single flute tool (you can make them from the broken Harvey end mills).
 
Are you using a router, or a HF mill converted to CNC or are you using a real machine tool? It makes a big difference in tool life.
 
Guys, thx for your replies.
Kenton: it is a CNC Masters Supra (?) mill. It’s a Bridgeport clone converted to CNC.
Rick Finsta: what is high feed milling? Profile ramp? My step down now is 1/3 of cutter diameter.
Thx.
 
Beginner CNC machinist here. Trying to cut 1/8" slots in 1/8" cold rolled steel. Not going well.

Using 4 flute carbide EM, 1/4" flute length. 4000 RPM, .042 DOC, .0003 feed/tooth. Based on info from Harvey tool site.

I can ramp in OK, but attempt today the cutter broke after about a 1/4" into slot.

Thinking i need to reduce the DOC. Even with the small feed/tooth the cutter may be loading up? I'm using a mist cooler.

I've had some success with a 3 flute. Maybe it was just luck. Thinking 4 flute should be stronger.

Please give me your suggestions.

Thx.

Marty

First of all, there is no such thing as "cold rolled steel". You have hot rolled and cold formed. What type of cold formed steel? There are many varieties with substantial differences. That is why 12L14 was mentioned. It is the best cuttingwise.
Secondly, your problem is sfpm. Are you at max rpm? Can you double it? What is the Length to diameter ratio of your cutter? If you are more than 2x the ratio you will have to drop your DOC.
 
Assuming that your cold rolled is in fact 1018 there seems to be something else going on. (I will say cold rolled, it is what I was taught, it is what everyone I know calls it, and I ain't gonna let COVID tell me what to do.)

If your CNC conversion has any motion control issues they will definitely cause small endmill to die a rapid death. Other issues that spring to mind are checking your tool runout and your tool pulling or slipping in your tool holder. Your speeds, feeds and cut depths are about where I would start on the spindle speed limited Proto-Trak I run at work.

Edit: if your ramp angle is too steep you could be damaging your cutting edges before you even get a chance to start cutting, causing your rapid tool failure.
 
If the tool has square corners that's a problem. Bigger radius the longer it lasts in steel.

My biggest issue when using 1/8" and smaller endmills is runout. I have bigger machines, rarely run anything under a 1/2" endmill. It's not unusual for me to run an 1/8" EM in a straight shank collet holder in a 50 taper holder. Easy to get a couple thou runout out at the endmill and the tool does about what you experience.

For a full width slot I don't usually take more DOC than 50% of the diameter to start with. Once the process is proved I'll squeak that up if there's room.
 
Guys, thx for your replies.
Kenton: it is a CNC Masters Supra (?) mill. It’s a Bridgeport clone converted to CNC.
Rick Finsta: what is high feed milling? Profile ramp? My step down now is 1/3 of cutter diameter.
Thx.

High Feed milling uses special tools with a larger radius than the tool diameter allows, and geometry that puts cutting forces axially up into the spindle and down into the workpiece. You take very large chiploads at high SFM and very low depth of cut and very large stepover. They don't remove material like HSM (high speed machining, where you go as deep as possible and take very small stepovers) but it is a very reliable process for slotting, long stickouts, sketchy setups, etc. They are great, but expensive.

On that type of machine, I would suggest you look at a bullnose 4-5 flute 3mm diameter tool with a reduced shank and very short flute length, and then ramp profile the part with a <1.5-2 degree angle or no more than 1/4 times the tool diameter total depth per pass. By profile ramping with a smaller tool than the slot width you can get away with a little more runout and you also can get better chip evacuation and less recutting.
 
Guys, thx for your replies.
Kenton: it is a CNC Masters Supra (?) mill. It’s a Bridgeport clone converted to CNC.
Rick Finsta: what is high feed milling? Profile ramp? My step down now is 1/3 of cutter diameter.
Thx.

I'd expect some backlash on that type of machine; you'll have to cut your parameters down significantly from the manufacturer's recommendations.
 
sample.jpg
Here is pic of my sample cutting program i did tonight. It encompasses all the features i'll need to do on the real template, aside from the slots will be much longer. The circle on the right i can ramp in OK, as well as the rectangle feature on the left. 1/8" hole at the top i can plunge in. The slot starts from the circle. I changed the program so the slot is taken in 4 passes. Cutter broke half-way through the 4th pass.

top burr.jpgtop burr2.jpg
Notice the big burr. I think the cutter is loading up. I would think a fresh cutter at these light cuts shouldn't create any burr like this. Looking at the broken cutter there appeared to be some material slightly stuck in the flutes. I could scrape it out, but had to work at it.

bottom burr.jpg
This is bottom side of sample, showing burr.

Guys, i appreciate your help with this. Please keep suggestions coming.
Marty
 
Hi, not a CNCer but if you REALLY do mean 0.0003"/tooth that cutter is trying to RUB its way thro' .. no wonder it broke! Try 0.002" per tooth or 0.003" which I suspect was really the recommendation.
 








 
Back
Top